Hello, I am using dsmcFoam to simulate a cold gas thruster that vents to a near vaccum. I used the supersonic wedge as my basis and adjusted the initial conditions for my problem. The geometry is just three concentric cylinders of growing diameter. The first cylinder having a inlet on its face and the final cylinder having an outlet on all faces except the area that interests with the middle cylinder. I am able to intialize and run the program, but when it comes to running the dsmcFieldsCalc, it breaks down. This is the error message that I recieve when I try running the command: Small value (min(mag(rhoNMean)) [0 -3 0 0 0 0 0] 9.99e-301) found in rhoNMean field. Not calculating dsmcFields to avoid division by zero. Has anyone come across this problem before and can explain how they fixed this? Thanks, yc

Yellow / vinz this happens in the very low density regions. (In paraview you can identify these cells using threshold whilst viewing the density fields.)
I had a similar problem and used some scripting as a quick fix. If you havent resolved the issue since your last message, post your case and i'll check if i can help.

1. I use the OpenFOAM version 2.2.1
2./3. I use the the wedge15Ma5 dsmc tutorial as base for my simulations
I took the simulation case and adapted it to an extern built mesh which I've imported to OpenFOAM without any failures in checkMesh. It looks like a windtunnel with inlet, outlet, walls and the geometry inside the windtunnel. As in the wedge15Ma5 tutorial i made the sides of the windtunnel to the "flow" region with "patch" and the geometry itself as the "obstacle".

With this i do the dsmcInitialise where particles are inserted and then I do dsmcFoam. But when doing the dsmcFieldsCalc there's always the mentioned failure message.

4. It's "only" a windtunner with an object inside it. So yes I can or anybody can built it quickly. (e.g from motorbike tutorial)

I'm not very familiar with these solvers. But I've found the file "discreteMethods/dsmcFoam/README" in the "tutorials" folder, which has some crucial information on what fields are used by this solver.

Beyond this, please provide a simple case that reproduces this problem. That way it'll take me considerably little time to try and diagnose the problem. Otherwise, don't expect me to give any answers on this before July 2014

I think I solved the problem. When you look at the file "discreteMethods/dsmcFoam/README" as you've said: [...]"setting zeroGradient boundary conditions on walls" [...] for iDof, internalE, linearKe, momentum, rhoM and rhoN.
I changed the originally "calculated" for my wall to zeroGradient and the dsmcFields-calculation works and i get overallT, UMean and so on...

I don't know exactly why there was calculated because these parameters are only relevant for cell data but now it works. If anybody does have some hints, please answer

I changed the originally "calculated" for my wall to zeroGradient and the dsmcFields-calculation works and i get overallT, UMean and so on...

I don't know exactly why there was calculated because these parameters are only relevant for cell data but now it works. If anybody does have some hints, please answer

It's somewhat simple to explain:

"zeroGradient" means that the patch imposes that the derivative must be zero, therefore there is a constraint in the boundary that will make the field values in cells adjacent to the patch to bend the flow in order to make the first derivative equal to zero. Note: this is usually necessary in situations where the equations need a constraint on a boundary, in order to be able to find a solution.

"calculated" means that anything that goes through the patch is inferred from the adjacent cells, without further restrictions. As you've mentioned, this is usually used in situations where either only the cell data is relevant or if the fields are fully calculated based on other fields.